Getting Started with VisualMill Version 4.0. VisualMill. The Solid/Surface/STL Model Manufacturing System. MecSoft Corporation

Transcription

1 Getting Started with VisualMill Version 4.0 VisualMill The Solid/Surface/STL Model Manufacturing System MecSoft Corporation 0

2 End-User Software License Agreement This MecSoft Corporation's VisualMill End User Software License Agreement that accompanies the VisualMill(TM) software product ( Software ) and related documentation ("Documentation"). The term "Software" shall also include any upgrades, modified versions or updates of the Software licensed to you by MecSoft. MecSoft Corporation grants to you a nonexclusive license to use the Software and Documentation, provided that you agree to the following: 1. USE OF THE SOFTWARE. You may install and use one copy of the Software on a single computer in a single location on a hard disk. 2. COPYRIGHT. The Software is owned by MecSoft Corporation and its suppliers. The Software s structure, organization and code are the valuable trade secrets of MecSoft Corporation and its suppliers. The Software is also protected by United States Copyright Law and International Treaty provisions. You must treat the Software just as you would any other copyrighted material, such as a book. You may not copy the Software or the Documentation, except as set forth in the "Use of the Software" section. Any copies that you are permitted to make pursuant to this Agreement must contain the same copyright and other proprietary notices that appear on or in the Software. You agree not to modify, adapt, translate, reverse engineer, de-compile, disassemble or otherwise attempt to discover the source code of the Software. Trademarks shall be used in accordance with accepted trademark practice, including identification of trademark owner s name. Trademarks can only be used to identify printed output produced by the Software. Such use of any trademark does not give you any rights of ownership in that trademark. Except as stated above, this Agreement does not grant you any intellectual property rights in the Software. 3. TRANSFER. You may not rent, lease, sublicense or lend the Software or Documentation. 4. LIMITED WARRANTY. MecSoft Corporation warrants to you that the Software will perform substantially in accordance with the Documentation for the thirty (30) day period following your receipt of the Software. To make a warranty claim, you must notify MecSoft Corporation within such thirty (30) day period. If the Software does not perform substantially in accordance with the Documentation, the entire and exclusive liability and remedy shall be limited to either the replacement of the Software or the refund of the license fee you paid for the Software. MECSOFT CORPORATION AND ITS SUPPLIERS DO NOT AND CANNOT WARRANT THE PERFORMANCE OR RESULTS YOU MAY OBTAIN BY USING THE SOFTWARE. THE FOREGOING STATES THE SOLE AND EXCLUSIVE REMEDIES FOR MECSOFT CORPORATION S OR ITS SUPPLIERS BREACH OF WARRANTY. EXCEPT FOR THE FOREGOING LIMITED WARRANTY, MECSOFT CORPORATION AND ITS SUPPLIERS MAKE NO WARRANTIES, EXPRESS OR IMPLIED, AS TO THE NON-INFRINGEMENT OF THIRD PARTY RIGHTS, MECHANTABILITY, OR FITNESS FOR ANY PARTICULAR PURPOSE. IN NO EVENT WILL MECSOFT CORPORATION OR ITS SUPPLIERS BE LIABLE TO YOU FOR ANY CONSEQUENTIAL, INCIDENTAL OR SPECIAL DAMAGES, INCLUDING ANY LOST PROFITS OR LOST SAVINGS, EVEN IF A MECSOFT CORPORATION REPRESENTATIVE

3 Getting Started with VisualMill HAS BEEN ADVISED OF THE POSSIBLITY OF SUCH DAMAGES OR FOR ANY CLAIM BY ANY THIRD PARTY. Some states or jurisdictions do not allow the exclusion or limitation of incidental, consequential or special damages, or the exclusion of implied warranties or limitations on how long an implied warranty may last, so the above limitations may not apply to you. To the extent permissible, any implied warranties are limited to thirty (30) days. This warranty gives you specific legal rights. You may have other rights which vary from state to state or jurisdiction to jurisdiction. For further warranty information, please contact MecSoft Corporation s Customer Support. 5. GOVERNING LAW AND GOVERNING PROVISIONS. This Agreement will be governed by the laws in force in the State of California excluding the application of its conflicts of law rules. This Agreement will not be governed by the United Nations Convention on Contracts for the International Sale of Goods, the application of which is expressly excluded. If any part of this Agreement is found void and unenforceable, it will not affect the validity of the balance of the Agreement, which shall remain valid and enforceable according to its terms. You agree that the Software will not be shipped, transferred or exported into any country or used in any manner prohibited by the United States Export Administration Act or any other export laws, restrictions or regulations. This Agreement shall automatically terminate upon failure by you to comply with its terms. This Agreement may only be modified in writing signed by an authorized officer of MecSoft Corporation. 6. U.S. GOVERNMENT RESTRICTED RIGHTS Use, duplication, or disclosure by the government is subject to restrictions as set forth in subparagraph (c) (1) (ii) of The Rights in Technical Data and Computer Software clause at DFARS or subparagraphs (c) (1) and (2) of Commercial Computer Software Restricted Rights at 48 CFR , as applicable. Manufacturer is: MecSoft Corporation, 17905, Sky Park Circle, Suite N, Irvine CA , USA. Unpublished - rights reserved under the copyright laws of the United States. MecSoft Corporation 17905, Sky Park Circle, Suite N Irvine, CA VisualMill is a registered trademark of MecSoft Corporation , MecSoft Corporation Trademark credits Windows is a registered trademark of Microsoft Corporation Pentium is a registered trademark of Intel Corporation Parasolid is a registered trademark of Unigraphics Solutions SolidWorks is a registered trademark of SolidWorks Corporation Solid Edge is a registered trademark of Unigraphics Solutions Rhino is a registered trademark of McNeel & Associates. 2

4 Version 4.0 Table of Contents Welcome to VisualMill... 6 About This Guide... 6 VisualMill Configurations... 6 Computer Requirements... 7 Installing VisualMill... 7 Installing the VisualMill Security Key... 7 Security Key Problems... 8 VisualMill Installation Folder... 8 Running VisualMill... 9 Registering VisualMill... 9 VisualMill Display VisualMill User Interface Typical Scenario Programming the Workflow Machining Operations Axis Operations ½ Axis Operations Drilling Operations Fourth Axis Operations Tutorial 1: 3 Axis Milling The File Toolbar Loading a Part Model View Toolbar Creating the Stock Browser Geom Tab Mops Tab Tools Tab Creating Tools Setting Feeds and Speeds

5 Getting Started with VisualMill Customizing Feeds and Speeds Status Bar Creating the Horizontal Roughing Toolpath VCR Toolbar Simulating the Horizontal Roughing Toolpath Creating the Pre-Finish Toolpath Creating the Pencil Tracing Toolpath Creating the Finish Toolpath Post-Processing Set Post Options Post Processor Generator Post-Processor Problems Tutorial 2: 2½ Axis Milling Operations Creating Tools and Stock Creating Regions Selecting Regions Multiple Regions Creating Toolpaths Clearance Plane Adjusting the Regions Replacing the First Toolpath Modifying Toolpath Parameters Toolpath Editing Tutorial 3: Drilling Operations Tutorial 4: 4 th Axis Machining Operations Creating Fourth Axis Toolpaths Cutting Strategy Measurement Toolbar Setting the Machine Zero Setting the Rotation Axis Creating the Parting Plane Creating 3 Axis Roughing Toolpaths

6 Version 4.0 Creating 4 th Axis Indexed Mode Finishing Operations Creating 4 th Axis Continuous Mode Finishing Operation Additional Topics Creating Surfaces Knowledge Base Where to go for more help

7 Getting Started with VisualMill Welcome to VisualMill Welcome to VisualMill and thank you for choosing one of most powerful and easy to use Solids/Surface/STL manufacturing packages on the market today. VisualMill is a unique, Windows-based, CAM product that seamlessly integrates toolpath generation and cutting simulation/verification, in one package that is both easy and fun to use. VisualMill s machining technology capabilities enable you to produce toolpaths that you can send to the machine with utmost confidence. A simple and well-planned user interface makes VisualMill suitable for use on the shop floor, working in conjunction with your existing CAD/CAM/CNC system. Solid models, surface models and faceted models can be imported into VisualMill, and a wide selection of tools and toolpath strategies to can be defined when generating toolpaths. These toolpaths can then be simulated and verified, and finally post-processed to the controller of your choice. About This Guide This guide is designed to introduce first-time users to VisualMill 4.0. The first part describes aspects of the user interface, machining strategies, and milling types. This is followed by several tutorials designed to familiarize you with the main features of VisualMill. In addition to the information provided in this guide, see the context-sensitive online help for more comprehensive explanations. You can also look at the models included in the Tutorials folder. VisualMill Configurations VisualMill 4.0 comes in two configurations - VisualMill Basic and VisualMill (standard configuration). VisualMill Basic is a general-purpose machining program targeted at the typical machinist. It is ideal for the rapid-prototyping, general machining, hobby and educational markets. The standard product is an advanced version, suitable for mold, die and tool making, woodworking, and other complex applications. This configuration is suitable for machinists with sophisticated manufacturing requirements. Both configurations support 2½ and 3 axis milling, as well as drilling. The standard version also supports 4 th axis milling. In addition, both versions can import Rhino, STL, IGES, DXF/DWG, VRML, and Raw Triangle files. The Parasolid interface add-on module includes the Parasolid kernel. This enables you to import Parasolid geometry data from the native design files of any Parasolid-based CAD system, as well as SolidWorks and Solid Edge files. 6

8 Version 4.0 Computer Requirements Intel Pentium compatible computer Windows NT, 95, 98, 2000, ME, or XP with at least 64 MB RAM. OpenGL-compatible graphics card, displaying at least 64,000 colors Approximately 50 MB of hard disk space. Installing VisualMill To install VisualMill software, follow these instructions: Windows NT 1. Insert the CD-ROM into the CD_ROM drive. 2. Go to the Program Manager and select Run from the File menu. 3. In the Command Line box, enter D:\setup (where D is the letter of your CD-ROM drive) and follow instructions. Windows 95, 98, 2000, ME, and XP 1. Insert the CD-ROM Disk into the CD_ROM drive. 2. The setup program will automatically launch once the computer detects the CD. 3. Follow the setup instructions. Installing the VisualMill Security Key VisualMill 4.0 ships with a hardware security device called the security key (or dongle ). This is either a 25-pin connector that connects to the parallel port of your computer, or a USB key that plugs into any USB port on your computer. If you have any other device, such as a printer, connected through the parallel port, disconnect it and connect the VisualMill security key. Then reattach the connector of the original device on top of the security key; the device will continue to operate as before. VisualMill will not operate correctly if the security key is not connected to the computer! 7

9 Getting Started with VisualMill Security Key Problems If you have installed the dongle but VisualMill is not running properly, try restarting your computer. If that still does not work do the following: 1. For Windows NT / 2000 / XP, double-click on the setupx86.exe icon found in the Win_NT folder in the VisualMill installation folder (see the section below that describes the installation folder). For Windows 95 / 98 / ME, double-click on the sentw9x.exe icon in the Win_9x folder. 2. Select Functions / Remove Sentinel driver and click OK. 3. Double-click on the RainbowInstaller.exe icon in the VisualMill 4.0 folder, then click OK. 4. Restart your computer. You can also download the Combo Installer from the Rainbow website ( and run the installation program. This will automatically install the drivers necessary for the proper operation of your security key. If the above method does not work, download the Sentinel Medic from the Rainbow website ( Install it and run SproMedic.exe. Click Find SuperPro and send the following information that appears on the screen to support@mecsoft.com, so that we can locate and fix your specific problem: 1. System Driver Info 2. Status 3. Description 4. Medic Says VisualMill Installation Folder VisualMill installation creates a main installation folder whose name and location you can specify during the installation process (or accept the default location of C:\Program Files\MecSoft Corporation\VisualMill 4.0). This folder contains the VisualMill executable and *.dll files. There are also several subfolders in the installation directory: Data: Contains tool library files - DefaultEnglishTools.txt and DefaultMetricTools.txt. These files can be used as they are, or you can use them as templates and customize them with your own data. You will also find a speeds/feeds & material library file called FEEDSPEEDS. For more information on how to modify these tool library files, please refer to VisualMill s online help. Examples: Contains various example files that you can experiment with. There are files from other CAD systems you can import, as well as VisualMill files (*.vmp). The *.vmp files contain saved machining operations that you can study and modify. Help: Contains the online help files used with VisualMill. You can open these files directly from this folder, or access them within VisualMill. 8

10 Version 4.0 Posts: Contains the standard set of post-processor (*.spm) files. Additional post-processor files can be obtained from MecSoft Corporation. If you receive additional *.spm files, be sure to place them in this folder, so that VisualMill will recognize them. Schema: Contains all the necessary files for loading Parasolid and Parasolid-based products, such as SolidWorks and SolidEdge files. Tutorials: Contains a tutorial and several part files to help first-time users get familiar with VisualMill. These are similar to the tutorials presented in this guide, in onscreen format. To launch these tutorials, open the VisualMill4.0Tutorials.chm file, and use the table of contents or arrows to browse through the steps. WIN_9x and WIN_NT: Contains the necessary files for the proper functioning of the hardware security key (dongle). Running VisualMill Click on the Windows Start button and select Programs. Point to the program group containing VisualMill. The name of this program group will be VisualMill 4.0, unless you specified otherwise during setup. Once you locate the program group, select it and then select VisualMill 4.0. Registering VisualMill After installation, you can run the full VisualMill version 50 times or for 30 days without registering the product. After this period, VisualMill will operate only in demo mode, without the ability to save part files or output toolpaths. When VisualMill is invoked, you will see the Enter License Code window. 9

11 Getting Started with VisualMill The Tries Left field indicates the number of times you can run VisualMill before it starts operating in demo mode. To obtain license codes you must register the product using the Web form available at If you have purchased the product directly from MecSoft Corporation, you will have to provide the purchase invoice number before you can be licensed. If you have purchased the product through an authorized VisualMill reseller, please obtain the license codes from your reseller. In addition to this information make sure you also provide the Dongle ID that is shown on the registration screen. You can also access this form from within VisualMill by selecting Help / Register VisualMill. VisualMill Display If you are experiencing problems with the way VisualMill appears on the screen, try the following: For Windows 98, ME, 2000 and XP: Right-click anywhere on the desktop and select Properties from the menu. 2. Open the Settings tab and click Advanced. 3. Open the Troubleshoot or Performance tab and set Hardware acceleration to None.

12 Version 4.0 If you are still having problems, reinstall the video drivers of your video card. Or you can try another video card to see if the problem is specific to your card. If VisualMill opens as a minimized window and closes when maximized (this happens on rare occasions, typically on computers with defective display cards), it is probably due to bad window coordinates stored in your computer s registry. Try the following to eliminate this problem: 1. Press Windows + R button. 2. Type in regedit and click OK. 3. In HKEY_CURRENT_USER / Software, delete the VisualMill4.0 entry. 11

13 Getting Started with VisualMill VisualMill User Interface VisualMill adheres to the Windows standard for user interface design. All functions can be accessed from the menus, and common functions are accessible via toolbar icons. Most user interface settings are modal - VisualMill remembers these settings and they remain active in subsequent operations unless you change them. The main VisualMill user interface objects are described below: File toolbar: Loads and saves part files Machining toolbar: Provides steps to create toolpaths VCR toolbar: Simulates material removal Input toolbar: Used when you need to enter values manually Browser: Displays geometry, machining operations, and tools View toolbar: Tools to show and hide components, change view, zoom, pan, etc. Status Bar: Displays status of tool, units, snaps, and cursor location Notes: There are additional toolbars you can display by selecting View / Toolbars. 12

14 Version 4.0 VisualMill Workflow The manufacturing process aims to successively reduce material from the stock model until it reaches the final shape of the designed part. To accomplish this, the typical machining strategy is to first use large tools to perform bulk removal from the stock (roughing operations), then use progressively smaller tools to remove smaller amounts of material (pre-finish operations). When the part has a uniform amount of stock remaining, a small tool is used to remove this uniform stock layer (finish operations). Load Part & Stock Create Roughing Operations Simulate Material Removal Create Pre-Finish Operations Create Finishing Operations Output Toolpaths to Machine This machining strategy is what you program using VisualMill. You can also simulate material removal to visualize how the stock model will look at any time during the process. This provides valuable feedback that can help you choose the most appropriate machining strategy. 13

15 Getting Started with VisualMill Typical Scenario Rough machining can be done by Horizontal Roughing (3 axis) or Pocketing (2½ axis) operations, using a relatively large flat end mill or an end mill with a corner radius. These rough operations can be followed by subsequent roughing operations, either using the same tool or a smaller tool. The part can then be pre-finished by using Parallel Finishing or Horizontal Finishing (3 axis) or Profiling (2½ axis). Pre-finishing and finishing operations typically use ball end mills, with or without a side angle. For complex 3D parts, additional finish operations may be necessary. For example, Parallel Finishing operation can be defined using a small ball tool with a fine stepover value. Once all of the operations are completed, you can go back and review the operation sequence, re-order and/or change operations if desired, simulate the material removal, and post-process the toolpaths. The browser can be used to manage these operations. Another powerful feature included in VisualMill is that of a Knowledge Database or K-Base. After creating an operation sequence for one part, you then save the operations and apply the same set of parameters and operation sequence to another part. This feature allows even novice users of VisualMill to machine parts quickly and easily. Programming the Workflow Once the part is loaded, the typical workflow is reflected in the layout of the icons in the Machining toolbar. Note: This toolbar is slightly different in VisualMill Basic. The steps are described below, and are demonstrated in the tutorials. Set Cutting Direction: Defines the side of the geometry to cut. Set Machine Zero: Aligns the part and stock geometry relative to the machine coordinate system. Set Table Rotation Parameters: Defines machine table rotation axis and rotation center for use in 4 th axis milling. Create/Load Stock: Provides several methods for creating (or loading) the geometry representing the raw stock from which the part will be machined. 14

16 Version 4.0 Locate Part Within Stock: Positions the part geometry within the stock. For example, you can align the top face of the part with the top face of the stock. Create/Select Tool: Opens a window in which you can define all the tools that will be needed in the machining operations. Set Feeds/Speeds: Defines the feed and speed rates for cutting, rapid, engage, and retract tool motions. Clearance Control: Sets the level above the part for safe rapid tool motion. Select Regions: Provides several methods for selecting curves that will act as machining boundaries. 3 Axis Machining: Operations in which the tool can move in all three directions. 2½ Axis Machining: Operations in which the tool can move in X and Y only, at set Z levels. Drilling: Drilling, tapping, and boring operations. 4 th Axis Machining: Operations in which the tool can move in all directions, and the machine table can rotate. Not available in VisualMill Basic. Toolpath Editor: Opens a window in which you can edit any line of toolpath code, insert special machine control commands, and make changes on groups of tool motions. Not available in VisualMill Basic. Post Process: Sends the toolpath code to the machine. Machining Operations There are two major classes of machining operations that can be created in VisualMill - milling and drilling. Milling operations are used to mill out material to form shapes. Drilling operations are used to create holes. Both classes are essential in any manufacturing industry. Milling operations can be categorized as 3 axis, 2½ axis, and 4 th axis milling. 3 Axis: The tool can move simultaneously in all three directions. 2½ Axis: The tool can move in X and Y directions, while the Z level is fixed at set locations. 4 th Axis: Rotates the machine table in order to machine parts that cannot be machined with simple 2½ axis or 3 axis operations. These categories, and the available operations, within them are described in the sections to follow. 15

17 Getting Started with VisualMill 3 Axis Operations In this type of machining, the tool can move simultaneously in all three axes. This is appropriate for parts that have complex, curved, and non-vertical surfaces. A typical machining scenario would be to first use Horizontal Roughing, the pre-finishing using Parallel Finishing and/or Horizontal Finishing. Once the part is at near net shape then fine detailed finishing could be performed by any of the re-machining or the region-based projection methods. The available 3 axis operations are shown and described below. Note: Only Horizontal Roughing and Parallel Finishing are available in VisualMill Basic. 16

18 Version 4.0 Horizontal Roughing This is VisualMill s principal method of roughing, also knows as waterline or constant Z cutting, in which the material is roughed out in horizontal layers. This type of machining is very efficient for removing large volumes of material, and is typically performed with a large tool. Roughing is typically followed by semi-finishing or finishing toolpaths. Both part and stock geometry are used to determine the regions that can be safely machined. Three types of cutting patterns are available: Linear (parallel, zigzag lines), Stock Offset (spiral pattern within stock and part), and Part Offset (spiral pattern outside the stock and outside the part). Tool motions are shown for single Z levels in the pictures below. Horizontal Roughing Linear Horizontal Roughing Stock Offset (Pocketing) 17

19 Getting Started with VisualMill Plunge Roughing Not available in VisualMill Basic Horizontal Roughing Part Offset (Facing) Sometimes called drill roughing, the tool can cut in the Z direction only, not in X and Y. The tool makes a series of overlapping plunges to remove cylindrical plugs of material. 18

20 Version 4.0 Horizontal Re-roughing Not available in VisualMill Basic This is used to create toolpaths in areas that were not machined by previous operations. Unmachined areas are determined by comparing the part to the stock remaining after the previous operation. Machining is performed in constant Z levels, one of which is shown below: Plunge Re-roughing Not available in VisualMill Basic Similar to Horizontal Re-Roughing, this method uses plunge motions to machine areas that were not machined by previous operations. 19

21 Getting Started with VisualMill Parallel Finishing This is an efficient method of finishing or pre-finishing, typically used when part surfaces are relatively flat. A 2D linear zigzag pattern is generated on the XY plane above the part geometry. The tool moves along this cut pattern, following the contours of the part geometry below. Pocket Finishing Not available in VisualMill Basic This method is used for pre-finishing and finishing of pockets with sculpted bottoms and/or sides. The pockets are defined by regions, and successive inner offsets of these outer regions are generated. The tool moves along these offset curves while following the contours of the part below. 20

22 Version 4.0 Horizontal Finishing Not available in VisualMill Basic This method is used for pre-finishing or finishing in constant Z levels, typically used when the part has large vertical surfaces and when Parallel Finishing will not yield satisfactory results. Pencil Tracing Not available in VisualMill Basic Used either for roughing, re-machining, or cleanup, the tool is driven along valleys and corners of the part. The system identifies all double contact or bi-tangency conditions based on the tool radius. It then creates cutting paths along these locations. When used as a roughing operation, valleys and corners are relieves so that subsequent operations will not encounter large amounts of material in these regions, thereby reducing tool deflection and wear. When used as a cleanup operation, scallops that remain after finishing operations are removed. 21

23 Getting Started with VisualMill Valley Re-machining Not available in VisualMill Basic This is used to machine corners and valleys that were inaccessible in previous finishing operations. Plateau Machining Not available in VisualMill Basic This method machines the tops of flat areas areas that are within a specified angle from horizontal. This is typically used to re-machine areas that remain unmachined after a Horizontal Roughing or Horizontal Finishing toolpath. 22

24 Version 4.0 Parallel Hill Machining Not available in VisualMill Basic This method machines steep areas. These are areas that are within a specified angle from vertical. This method is typically used when a Parallel Finish toolpath leaves scallops on steep areas. The cut angle is adjusted so that machining is always normal to the steep areas, thereby leaving minimal scallops. Horizontal Hill Machining Not available in VisualMill Basic Similar to Horizontal Finishing, this method machines in constant Z levels. However, machining can be restricted only to areas in the part that are steeper than a user-defined steepness angle. 23

25 Getting Started with VisualMill Radial Machining Not available in VisualMill Basic This method is used as a finishing operation for areas that have annular pockets. You must specify one or more machining regions; the tool moves radially from the centroid of these regions. Spiral Machining Not available in VisualMill Basic This method is used for finishing areas that have circular or near-circular characteristics, such as pocket bottoms. You must specify one or more machining regions; the tool moves in a spiral pattern based on the centroid of these regions. 24

26 Version 4.0 Curve Machining Not available in VisualMill Basic Suitable for machining isolated areas or shapes, this method machines along a curve. You must specify one or more machining regions, direction and cut pattern. The tool simultaneously follows the region and the contours of the part below. Between 2 Curves Machining Not available in VisualMill Basic Sometimes called flowline machining, this method machines between two open or closed curves. Using a pattern either parallel or normal to the curves, the toolpath makes a gradual transition from one curve to the other. This creates a blended toolpath that can be used to efficiently finish complex shapes. 25

27 Getting Started with VisualMill Reverse Post Milling Not available in VisualMill Basic This feature loads toolpaths from APT CL files and ISO standard G Code files. You can use these toolpath motions to project the tool onto part surfaces. You can also load an existing toolpath in order to simulate it in VisualMill. 2½ Axis Operations In 2½ axis toolpath, the tool can move in X and Y directions, but Z movements are limited to set levels. Because 2½ toolpaths do not relate to either part or stock geometry, machining regions must be selected; these define the boundaries of tool motions. This type of machining is useful for machining prismatic parts extrusions of curves along the Z axis. Because of its straight sides, a prismatic part can be machined by locking the tool at the first Z level, performing XY motions, then repeating for subsequent Z levels. Using this class of machining, you can machine parts that are defined only by 2D curves. 3D part geometry can be present, though it is not necessary. As with 3 axis operations, a typical machining operation would involve roughing then finishing. Unlike the more complex 3 axis parts, detailed finishing is typically not necessary for prismatic parts. Roughing 26

28 Version 4.0 is typically performed using a combination of Facing and Pocketing operations, and Profiling is used for finishing. The available 2½ axis operations are shown and described below. Note: Facing is not available in VisualMill Basic. Facing Not available in VisualMill Basic This method machines closed regions as if they were completely enclosing material to be removed. This means that the tool can approach the material from outside the outer regions, creating reverse pockets. This example uses multiple regions the rectangle is the outer region, and each letter is an inner region. Some letters have nested regions; these are treated as islands (areas to avoid). Note: The outer region should encompass the stock. You can easily create this type of region by selecting Curve / Bounding Region / Stock Bounding Region. 27

29 Getting Started with VisualMill The toolpath looks like the following: The stock simulation: 28

30 Version 4.0 Pocketing This method machines closed regions as if they were pockets - completely enclosed by inner and outer regions. The tool cannot go beyond the outer region, and cannot go within inner regions. This is unlike Facing, in which the outermost region is considered to enclose material to be removed. This example uses similar regions as the previous Facing example, but the outer region is within the stock limits. The toolpath looks like the following: The stock simulation: 29

31 Getting Started with VisualMill Profiling This method machines open and closed regions by tracing along one side of their contours. You can define offsets so that the tool makes multiple passes relative to the regions. Profiling can be used as a finishing operation after a Pocketing or Facing toolpath, or it can be used alone. Engraving Typically used for engraving text or logos on a finished mode, this method machines open or closed, 2D or 3D regions by tracing along the contours. This method is similar to Curve Machining, in which the tool is projected onto the part surfaces below the regions being followed. You can use a conical tool such as a drill tool for engraving. 30

32 Version 4.0 Drilling Operations These operations are used to create holes in the part, including drill holes, counter sunk holes and through holes. Tapped and bored holes can also be created. The following drilling operations are available: Note: Tapping, Boring, and Reverse Boring are not available in VisualMill Basic. Drilling The following drill cycles are available: Standard: Used for holes whose depth is less than three times the tool diameter. Deep: Used for holes whose depth is greater than three times the tool diameter, especially when chips are difficult to remove. The tool retracts completely to clean out all chips. Counter Sink: Cuts an angular opening at the end of the hole. Break Chip: Similar to Deep drilling, but the tool retracts by a set clearance distance. 31

33 Getting Started with VisualMill Tapping Not available in VisualMill Basic A Tap cycle is used to drill threaded holes in the part, clockwise or counter-clockwise. Boring Not available in VisualMill Basic A Bore cycle is used to form shapes inside a hole. The following boring cycles are available: Drag: The tool is fed to the specified depth at the controlled feed rate. Then the spindle is stopped and the tool retracts rapidly. No Drag: The tool is fed to the specified depth at the controlled feed rate. It is then stopped to orient the spindle, moved away from the side of the hole and then retracted. Manual: The tool traverses to the programmed point and is fed to the specified depth at the controlled feed rate. Then the tool stops and is retracted manually. Reverse Boring Not available in VisualMill Basic This is simply a Bore cycle in the reverse direction. The spindle is oriented to the specified angle and moves rapidly to the feed depth and moved to the part. The spindle is turned on and the cycle is started. 32

34 Version 4.0 Fourth Axis Operations Not available in VisualMill Basic Fourth Axis operations are used to machine parts that cannot be machined with simple 2½ axis or 3 axis operations. During 2½ and 3 axis milling, the tool remains vertical and the table is fixed. This means that areas of the part that cannot be accessed from above cannot be cut. There are generally two ways to use 4 th axis operations indexed or continuous mode. The Set Table Rotation Params command enables you to set the rotation axis and origin for the table. Indexed mode: Use 3 axis operations to mill one half of the part, flip the table using a Rotate Table command, and then mill the other half. You are not restricted to 180-degree rotations. Continuous mode: The part is rotated continuously so that the tool is always normal to the axis of rotation. This is useful for machining multi-sided parts. The available 4 th axis operations are shown and described below. 4 th Axis Parallel Finishing In this method, the tool is always normal to the axis of table rotation (continuous mode). The tool can move in all directions while the table rotates continuously. The tool motions can be parallel to or normal to the rotation axis. 33

35 Getting Started with VisualMill 4 th Axis Engraving Similar to 3 axis engraving, this method machines text or logos by following the contours of the selected regions. Continuous mode is also used here. 34

36 Version 4.0 Tutorial 1: 3 Axis Milling In this tutorial, you will create 3-axis milling toolpaths to manufacture a designed part. The stepped instructions are accompanied by explanatory and introductory text. Reading this text will help you understand the tutorial methodology and provide information about additional options available. However, if you prefer to work straight through the steps without any additional reading, look for the following symbol: Don t forget to save your work periodically! You may want to save the file under a different name so that the original file will be preserved. The File Toolbar Before beginning, the first commands you should know are on the File toolbar. These commands are used to load and save files, and can also be accessed from the File menu. New: Creates a new file. Open: Loads part geometry into VisualMill. This geometry is typically imported from other CAD formats. Save: Saves the current file as a *.vmp file. We recommend saving your work periodically, to avoid losing data. Loading a Part Model Part refers to the geometry that represents the final manufactured product. You can create parts within VisualMill, but it is more typical to import geometry created in another CAD system. You can import solid models of standard Parasolid XT format, or Stereo-Lithography (both ASCII and binary) format files. Surfaces can be imported from IGES or Rhino 3DM. Faceted (triangulated) models can be imported from VRML, Raw Triangle, DXF / DWG facet data, or Rhino Mesh. Non-faceted geometry, once imported, is immediately converted and stored as triangulated data. Imported geometry is stored internally as a VisualMill part file. This allows for much faster part loading time. 35

37 Getting Started with VisualMill To load a part: 4. Select File / Open, or click the Open Part File icon from the File toolbar. 5. From the Open dialog box, select the dumbells.vmp file from the Tutorials folder in the VisualMill installation folder. The imported part appears as shown below. Note: Depending on your settings, you may also see the browser, construction grid, coordinate axes, and/or regions. You can use the options in the View menu or View toolbar to adjust what appears. You can change the background color and color of the part by selecting Preferences / Color Preferences and clicking the relevant color box. The browser can be displayed or hidden by selecting View / Toolbars / Browser. 36

38 Version 4.0 View Toolbar The View toolbar is used for view and display manipulation. By default, it appears vertically along the left side of the screen, but you can dock it anywhere. Each of the view functions is described below: Zoom In: Doubles the displayed size. Zoom Out: Halves the displayed size. Zoom Box: Zooms in on an area you specify by defining a rubber-banded rectangle. Center View: Centers the view about a selected point. Fit View: Fits the entire part into display extents. Repaint View: Repaints, or refreshes, the view. Dynamic Pan View: Pans the view by holding and dragging the mouse. Dynamic Zoom View: Zooms the view by holding and dragging the mouse. Move the mouse up to zoom in, move the mouse down to zoom out. Dynamic Rotate View: Rotates the view by holding and dragging the mouse. The rotation follows the mouse movements as if there were an imaginary trackball at the center of the view. Dynamic Rotate View About Z: Rotates the view about the Z axis and the origin point, by holding and dragging the mouse. Top View: Displays the top view - the XY plane. Right View: Displays the right view - the YZ plane. Front View: Displays the left view - the XZ plane. 37

39 Getting Started with VisualMill Iso View: Displays the model in isometric projection. Hide Part Model: Toggles the display of part geometry. Shade Part: Toggles the display of part geometry between shaded and wireframe modes. Hide Stock: Toggles the display of the stock geometry. Reset Stock Color: Resets the stock color after simulation to the original color of the stock. During simulation, the cut stock takes on the Cut Stock color (defined in Preferences / Color Preferences). If you reset the stock color, only the results of the next toolpath simulation will be shown in the Cut Color. Hide Machining Regions: Toggles the display of regions. Display Grid: Toggles the display of the construction grid. Hide Toolpath: Toggles the display of the toolpath associated with the current machining operation. Display Next Z: Displays the toolpath for each level. This button is only active for horizontal milling operations. Hide Coordinate Axis: Toggles the display of the coordinate axes. Creating the Stock Stock represents the raw stock from which the part will be manufactured. Stock geometry can either be created within VisualMill or imported from an external file. You can import Parasolid XT solid models and STL solid models (ASCII and binary) for stock geometry. Surfaces can be imported from IGES or Rhino 3DM. Faceted (triangulated) models can be imported from VRML, Raw Triangle, DXF / DWG facet data, or Rhino Mesh. Stock can also be created within VisualMill by entering coordinates or as the bounding box of the part or a toolpath. You can also define stock as a uniform offset of the part geometry, to simulate casting or forging raw stock model. Note: You must define a stock model before creating Horizontal Roughing and Plunge Roughing operations. All other operations can be created without first creating a stock model. 38

40 Version 4.0 To create the stock: 1. Select Stock / Part Box Stock, or click Create/Load Stock from the Machining toolbar and select Part Box Stock. This option enables you to create a stock box that encloses all of the part geometry (bounding box). 2. In the Part Bounding Stock Box window, you can expand the bounding box by entering offset values. For the purposes of this exercise, do not enter any offsets. Click OK. 3. If you are asked whether you want to display the stock, click Yes. 4. The stock model is created. To display the stock, make sure the Hide Stock toggle icon in the View toolbar is not pressed. 39

41 Getting Started with VisualMill The stock is displayed as a box over the part. Its color can be set in the Color Preferences. Tip: Stock is used for simulation, and its display involves data-intensive rendering. This can slow down VisualMill s performance. Therefore, we recommend turning off the stock display when not needed. Browser The browser appears to the left of the screen by default, and can be displayed or hidden by selecting View / Toolbars / Browser. Like all toolbars, you can drag it to another location by clicking and dragging it by one of its corners. You can also resize it by dragging one of its sides. Standard Windows operations can be used here, when appropriate. You can drag and drop items to change their order, and Ctrl+C (copy), Ctrl+X (cut), and Ctrl+V (paste) can be used. Dragging an item outside the browser will delete it. Items can be renamed here as well. 40

42 Version 4.0 The browser contains the following three tabs: Geom Tab Not available in VisualMill Basic The geometry manager displays the three types of geometry that can be created and manipulated in VisualMill: Part, Stock and Regions. The first icon represents the Part. For an imported part, the full path is indicated. If the part consists of surfaces, each surface is represented as a Mesh. You can click on each mesh name to highlight its corresponding surface. The Stock icon indicates the type of stock. You can double-click to create a different type of stock, or right-click to or delete the stock or export it to an *.stl file. A red star next to this icon indicates that the work-in-progress stock model corresponding to this operation needs to be created. The last section is Regions. These are curves in the model that are used to define machining boundaries. You will work with regions in the next tutorial. 41

43 Getting Started with VisualMill Mops Tab Mops stands for Machining Operations. All toolpaths you create are listed here, in order of creation. Within each toolpath folder you can edit its various components, such as tool, regions, or cut parameters, by double-clicking the relevant icon. Right-clicking on a toolpath name provides several options, including simulation, generation, and post-processing. If you make any changes to a toolpath s parameters, the yellow folder icon for that toolpath will turn red. This indicates that the toolpath needs to be regenerated. Tools Tab This tab lists all tools currently defined in the file. If you have created machining operations, the toolpath will appear in the Tools tab underneath the tool it uses. 42

44 Version 4.0 You can rename and delete tools, but you cannot delete a tool that is used in a toolpath. Double-click a tool icon to edit its parameters. Creating Tools VisualMill supports ball mills, flat end mills, corner-radius or bull nose, and taper end mills, in addition to drills, taps and bores. For each tool you can specify standard APT parameters: diameter, corner radius, taper angle, flute length and tool length. Flute length is the cutting length, and Tool Length is the total length of the tool up to the tool holder. All defined tools can be viewed in the Tools tab of the browser. You can also save a set of tools to an external folder that can be loaded in other files. To create the roughing tool: 1. Select Tool / Create/Select Tool, or click the Create/Select Tool icon on the Machining toolbar. 2. In the Select/Create Tools window, click the Flat End Mill tab. Note: This window looks slightly different in VisualMill Basic. 43

45 Getting Started with VisualMill Leave the default values as they are and click Save as New Tool. The tool will be created and its name (FlatMill1, by default) will be displayed in the tool list. To create the pre-finishing tool: 1. In the Select/Create Tools window, click the Ball End Mill tab. 2. Again, accept the default tool parameters and click Save as New Tool. You have created the BallMill1 tool that has a diameter of 0.5 inches. 44

46 Version 4.0 To create the pencil trace tool: Pencil tracing is usually performed with a bull nose tool with a smaller diameter than the pre-finish tool. 1. While still in the Ball End Mill tab, change the tool diameter from 0.5 to 0.25 inches. 2. Change the tool name to BallMill2. 3. Click Save as New Tool. 45

47 Getting Started with VisualMill To create the finishing tool: Finishing is typically performed using a ball mill with a diameter much smaller than that of the prefinishing tool. 1. While still in the Ball End Mill tab, change the tool diameter to inches. 2. Change the tool name to FineFinisher. 3. Click Save as New Tool. 4. Click OK to close the window. 5. Now that all tools have been created, click the Tools tab in the browser. All the tools are listed. 46 If the file had tools already defined, they will be displayed here as well. But only the four tools you just created will be used.

48 Version 4.0 Note: You can double-click on any tool to open its definition window. This is an easy way to make changes, if needed. 6. A group of tools can be saved to a library file for future use. Select Tool / Save Tool Library. 7. In the default folder (should be Tutorials, which contains the part file), assign the name Dumbells_Tools. The default extension is *.csv (comma-separated values), which means the file can be opened and edited as a spreadsheet or in a text editor. Click Save. 8. Right-click on the Tools header in the browser and select Delete All. 9. To replace the tools, select Tool / Load Tool Library. Select the *.csv file you just saved, and the tools reappear in the file. Setting Feeds and Speeds You can set toolpath feeds and speeds and customize these settings for later use. The Set Feeds / Speeds icon on the Machining toolbar accesses these parameters. You can assign values for the following: Spindle Speed: The rotational speed of the spindle, in RPM. Cut Feed: The feed rate used when the tool is cutting, in inches per minute. Engage Feed: The feed rate used when the tool is approaching the part. By default this value is 75% of the Cut Feed. Retract Feed: The feed rate used when the tool is retracting from the part. By default, this is equal to Engage Feed. Transfer Feedrate: Specifies the feedrate of transfer motions (air motions). You can either use the Rapid setting of the tool, or set a custom feed rate. 47

49 Getting Started with VisualMill Customizing Feeds and Speeds You can customize the feeds and speeds based on the stock material, tool material, and operation type. Then your settings can be saved to a file for future use. A default feed / speed table is in the FEEDSPEEDS file (no extension), located in the Data folder. You can edit this file and then store your values in an ASCII external file. The format for this file is shown below: TYPE { STOCK_MATERIAL TOOL_MATERIAL SURFACE_SPEED UNITS FEED/TOOTH UNITS MACHINABILITY UNITS STOCK_MATERIAL TOOL_MATERIAL SURFACE_SPEED UNITS FEED/TOOTH UNITS MACHINABILITY UNITS... } Example: FaceMilling { aluminum-cast carbide 900 fpm in 4.0 ci/min/hp aluminum-cast hss 650 fpm in 4.0 ci/min/hp aluminum-plate carbide 900 fpm in 4.0 ci/min/hp aluminum-plate hss 650 fpm in 4.0 ci/min/hp } 48

50 Version 4.0 You can load values from this table by selecting Feeds/Speeds / Load Feeds/Speeds. Type, Stock Material, and Tool Material are parameters in the external file. The Surface Speed and Feed/Tooth values are calculated based on these fields. Tool Diameter and # of Flutes are taken from the currently active tool (if any) and are used to calculate Spindle Speed and Cut Feed. By changing parameters of the active tool, you can use this window as a feed/speed calculator. The current Cut, Engage, Retract, and Transfer Feeds are displayed in the top-right box. If you want to modify these values based on the calculated values on the left side, copy the values to the relevant fields on the right side and click OK to update. 49

51 Getting Started with VisualMill To set feeds and speeds: 1. Select Feeds/Speeds / Set Feeds/Speeds or click the Set Feeds/Speeds icon on the Machining toolbar. 2. Leave the spindle speed as is and change the Cut Feed to 30 in/min. Set the Engage Feed and Retract Feed to 20 in/min. Click OK. These feeds and speeds will be used during the post-processing of the toolpath. 50

52 Version 4.0 Status Bar The Status Bar, located at the bottom of the screen, is used to display information about the current activities. The left-most field displays the current command and any prompts or help information associated with this command. If you place the cursor over an icon, its description will appear here. The next field indicates the active tool, if any. The name of the tool, followed by the diameter and corner radius, is displayed. The next field indicates the progression of toolpath simulation ( Goto ), displaying the number of the motion being simulated. When the simulation is complete, the last motion number will be displayed. The next three fields (Snap, Ortho, and Osnap) display snap modes for point input. These fields can be turned on and off by clicking in them. Snap: Toggles the ability to snap to grid points. Ortho: In Ortho mode, all lines are horizontal or vertical. Osnap: Object snap - toggles the ability to snap to points on the model and on regions and curves. The second to last field displays the work units inches or mm. The last field shows the current location of the cursor as X, Y, Z coordinates. These values update as the cursor moves. Creating the Horizontal Roughing Toolpath In this type of toolpath, VisualMill uses stock geometry and part geometry to determine the safe machining region at each user-specified Z level. The safe machining region is the region in which the tool can safely traverse removing stock. Once this machining region is determined, a tool traversal pattern such as a zigzag or offset machining cut pattern can then be applied to remove stock. Note: For 3 axis milling, you can also create and activate regions that act as machining boundaries. An example would be if you wanted to machine only one surface; you could define a region around that surface so that no other areas will be milled. Regions are curves that already exist in the model, or curves you create within VisualMill. In the Geom tab of the browser, you will see that one region already exists in this file. Regions will not be used in Tutorial 1, since they are not required for 3 axis milling. However, they are required for 2½ axis milling, so you will learn about them in Tutorial 2. 51

53 Getting Started with VisualMill To create the horizontal roughing toolpath: 1. First you must activate the tool to be used. Select Tool / Create/Select Tool or click the Create/Select Tool icon on the Machining toolbar. 2. Select the Flat End Mill tab, pick FlatMill1 and click OK. FlatMill1 is now the active tool, and is listed in the Status Bar. 3. Select 3-Axis Milling / Horizontal Roughing, or click the 3-AxisMaching icon on the Machining toolbar and select Horizontal Roughing. The Horizontal Roughing window opens, in which you can set various parameters for the toolpath. 4. Click the Cut Parameters tab. At the top of the window are Global Parameters Intol, Outol, and Stock. Stock: The thickness of the layer that will remain on top of the part after the toolpath is complete. Roughing operations generally leave a thin layer of stock, but for finishing operations this value is zero. 52

54 Version 4.0 Intol and Outol are allowable deviations (tolerances) from the actual part geometry plus the Stock layer (if any). Intol: Inward tolerance - the maximum thickness of material that can be removed from the Stock layer. Outol: Outward tolerance - the maximum thickness of material that can remain above the Stock layer. 5. Leave the Global Parameters as they are, but change the Cut Direction to Mixed. This enables the tool to cut either up or down, so that the tool does not have to retract each time the direction changes. Minimizing the number of tool retractions creates a cleaner toolpath. 6. Click the Cut Levels tab and set the Bottom cut level to 0.0. (You must first check the box in order to activate the field.) 53

55 Getting Started with VisualMill 7. Leave the remaining parameters in the other tabs as they are, and click Generate, located at the bottom of the window. The window will disappear and an hourglass cursor will appear on the screen. When the calculation is complete, the roughing toolpath will appear. In this toolpath there are so many cut levels that the display is too dense for you to decipher much detail. It is helpful to view the toolpath one level at a time. 8. Click Display Next Z on the View toolbar. All Z levels are listed, and you can click the desired level to see its tool movements. 9. Close the Z Level Display window. 54

56 Version Look in the Mops tab of the browser, where you can see the toolpath you just created. VCR Toolbar The VCR commands are used for toolpath simulation. The VisualMill simulator enables you to view your toolpath in action, reflecting what the actual model would look like after machining. Simulation can also be used to catch errors. The cut stock can also be visually compared with the part model to indicate any areas of uncut or overcut material. For simulation to work, you must have stock geometry defined, and the stock must be displayed. Simulate: The simulation will be run for the entire toolpath, and the end result of the material removal will be displayed. Simulate Until: Shows removed material for all operations up to and including the currently selected one. Step Increment: Controls the number of steps that are simulated each time you click Simulate Each Step. You can choose one of the numbers in the drop-down list or enter a number. Simulate Each Step: The simulation will be performed for a specified number of toolpath motions, specified in the Step Increment box. Simulate with Display: The entire simulation will be run in animation, including a symbol for the tool. 55

57 Getting Started with VisualMill Simulate with Display Each Z Level: Simulates the toolpath for each successive Z level. This is applicable only for machining methods that use multiple Z levels for machining, such as Horizontal Roughing and Pocketing. Compare Part/Stock: Performs a visual comparison of the stock model against the part model. You can color-code areas based on the amount of material remaining or overcut. Note: You can press the Esc key to interrupt the simulation. Simulating the Horizontal Roughing Toolpath Now that the first toolpath has been created, you can simulate it. There are two simulation models in VisualMill 3 axis and 4 axis. You can choose the simulation model by selecting Preferences / Machining Preferences. The 3 axis model is very fast. It uses a grid to represent the stock, so it can only be used for 2½ and 3 axis simulations (in which the bottom of the part is squared off). The 4 axis simulation is a true simulation (uses the true stock shape), and may therefore be slower than the 3 axis model. To simulate the toolpath: 1. Be sure you are using the 3 Axis Simulation Model. Verify this in Preferences / Machining Preferences. 2. Click Hide Toolpath on the View toolbar to clear the toolpath from the display. 56

58 Version On the View toolbar, make sure the Hide Stock icon is not pressed. You need to see the stock in order to see the simulation. 4. On the VCR toolbar, click the Simulate icon. This will start the simulation, which will stop when all of the tool motions have been processed. During the simulation you will see the count of the toolpath motions dynamically displayed in the Status Bar. Note: You can also try clicking Simulate Each Step to simulate smaller numbers of motions at once, Simulate with Display to see the tool moving while removing material, or Simulate with Display Each Z Level to see levels removed one at a time. Once the simulation is complete, the cut stock model will be displayed. This cut model can be used as input stock geometry for simulating the toolpath of subsequent machining operations. 57

59 Getting Started with VisualMill Tips: To get a better view during simulation, you can also turn off the display of the part. You can change the color of the cut stock by selecting Preferences / Color Preferences and clicking the color box for Cut Stock Color. Creating the Pre-Finish Toolpath Once the roughing toolpath is generated, a pre-finish toolpath can be created to remove the steps left by the roughing process, and to bring the stock closer to the part. There are several methods of generating pre-finishing toolpaths; in this exercise will use the Parallel Finishing method. To create the pre-finish toolpath: 1. Make sure both the stock and toolpath are displayed. 2. Open the Select/Create Tools window, click the Ball End Mill tab, and select BallMill1. Click OK to make this the active tool. (You could also double-click the tool name.) 3. Select 3 Axis Milling / Parallel Finishing, or use the 3 Axis Machining icon. We will use all default settings except for the stock value. Pre-finishing is typically done so that there is a uniform thickness of stock left on the part, to be removed by the final finish path. 4. Click the Cut Parameters tab, and enter in the Stock field. 58

60 Version Click Generate to calculate the toolpath. This toolpath uses a linear zigzag pattern. To simulate the pre-finish toolpath: 1. Turn off the toolpath display, but make sure the stock is displayed. Hide the part. 2. On the VCR toolbar, click Simulate Until. The results show how the stock will look after the pre-finishing toolpath is run. 59

61 Getting Started with VisualMill Creating the Pencil Tracing Toolpath Not available in VisualMill Basic. Basic users proceed to Creating the Finish Toolpath. In Pencil Tracing, VisualMill automatically determines all areas of the part where a tool would have more than one contact position. These areas are typically in valleys and corners. The tool is then moved along these areas to remove material. This is a very efficient method to stress-relieve corners and valleys before running a pre-finish toolpath. It can also be used as a cleanup operation to remove scallops left in these areas after finishing operations. Pencil tracing is typically performed with a ball end mill. To create the pencil tracing toolpath: 1. Display the toolpath, and make BallMill2 the active tool. 2. Select 3 Axis Milling / Pencil Tracing. 3. In the Pencil Trace Cut Parameters tab, set Stock to Leave all other parameters at their default settings. 60

62 Version Click Generate. Tip: Pencil tracing is typically performed with ball end mills. If there are any fillets in the model, make sure that the pencil tool radius is slightly larger than the maximum fillet radius. This ensures that the tool will be driven along all of the fillet surfaces. To simulate the pencil tracing toolpath: 1. Hide the toolpath and display the stock. 2. As you have probably noticed, after the simulation is complete the cut areas of the stock are colored using the specified cut color. On the View toolbar, click Reset Stock Color, which returns the entire stock to the original stock color. This gives a clear view of cut areas in subsequent cut simulations. 61

63 Getting Started with VisualMill 3. On the VCR toolbar, click Simulate. Notice how the pencil trace toolpath removes the scallops along the valleys of the part. Creating the Finish Toolpath In finish machining, all of the remaining stock is removed to create the final net shape. This example will use the Parallel Finishing method again. Finish machining is almost always performed with a ball end mill. Here we will use the final finish tolerance as well as use a very fine stepover value. To create the finish toolpath: 4. Activate the FineFinisher ball end tool. 5. Select 3 Axis Machining / Parallel Finishing. 62

64 Version The parameters are already set to finish tolerances, but we will change a few items: Change the Stock value from (used in the previous toolpath) to 0.0. This leaves no layer of stock over the resulting part. Change the Angle of Cuts to 90 degrees, relative to the previous pre-finish cuts. This will create a better finish on the part. Change the Stepover Control value from 25% to 10% of the tool diameter. This reduces the distance between passes, making for a better finish. 63

65 Getting Started with VisualMill 7. Click Generate. 8. Reset the stock color, and simulate. The final part is displayed, and in the Browser you can see all the toolpaths you created. 64

66 Version Click the Tool tab in the browser to see each tool, linked to the toolpath that uses it. Post-Processing Once the toolpath has been generated, it can be post-processed to a specific machine controller. VisualMill Standard comes with a set of post-processors to choose from. Each post-processor is represented by an *.spm file, all of which are located in the Posts folder under the VisualMill installation folder. You can post-process an individual toolpath, or all toolpaths at once. For an individual toolpath, rightclick on its name in the Mops tab of the browser and select Post. You can also click Post Process on the Machining toolbar. The entire list of toolpaths can be post-processed by right-clicking the root folder in the Mops tab and selecting Post All. 65

67 Getting Started with VisualMill Set Post Options Some post-processor options can be set by selecting Post Process / Set Post Options. By default, VisualMill performs interactive post-processing. In other words, VisualMill launches the post-processor and waits for the post-processor to complete. You can check Post Process in Batch Mode to tell VisualMill not to wait for the completion of the post-processor. You can also output the list files and display the selection dialog for each post processing operation. During interactive post-processing, VisualMill launches a text editor to display the output file. By default, Notepad is used, but you can specify a different program. 66

68 Version 4.0 Post Processor Generator You can select Post Process / Post Processor Generator to edit post processor parameters, and set up your own post-processors. Click a post processor to change or copy, and click Edit. The editable parameters can be found on the various tabs. To create a new post-processor, define the parameters and click Save As. A new *.spm file will be created in the Post folder. You can also output the toolpath in an APT standard Cutter Location (CL) file. APT is a widely accepted Numerical Control Machine standard. This CL file can then be used to create a machine specific post-processed output through any of the many commercially available APT post-processors. 67

69 Getting Started with VisualMill To create the post-processed output: In this exercise we will post-process all of the toolpaths at once. 1. In the browser, click the Mops tab. The toolpaths are shown here collapsed. 2. Right-click on the root folder (Machining Operations) to open the popup menu. Select Post All. 3. Browse to the desired output directory and assign a file name for the output. The default extension is *.nc. Then double-click on the post-processor you want to use (such as Fanuc 1). 68

70 Version When complete, the post output file will open in the default text editor (Notepad by default). This file contains all the G-code for your toolpaths. Note: You can post individual toolpaths by right-clicking on their name in the Mops tab and selecting Post. The Post-Process icon on the Machining toolbar can also be used. To post multiple toolpaths, select each toolpath while keeping Ctrl pressed, right-click, and select Post All. Post-Processor Problems If only two built in posts (APT CLS and Roland CAMM GL) are displayed in the selection dialog, then your Post folder is not set correctly. Try the following: 1. Click Browse on the Select Post Processor window. 2. Select the Posts folder located in the VisualMill installation folder. If nothing happens when the toolpath is posted, try the following: 1. Select Post Process / Set Post Options. 2. Make sure Show Selection dialog when Post Processing is checked. 3. Make sure Post Process in Batch Mode is not selected. 4. Make sure Output Listing Files is not selected. 5. Post the machining operations, making sure you are browsing to the Post folder in the VisualMill installation folder. For the output file at the bottom, make sure there is a valid file name (valid path). End of Tutorial 1! 69

71 Getting Started with VisualMill Tutorial 2: 2½ Axis Milling Operations This exercise uses the file spanner.vmp, located in the Tutorials folder. Use File / Open to load the part. This part is suitable for 2½ axis milling because it is prismatic it is a straight extrusion of curves in the XY plane. The solid geometry is not actually necessary for programming this part, but it is helpful when visualizing the process. Creating Tools and Stock Before any operations can be performed, you must define the milling tools and the stock geometry. To create the 2½ axis milling tools: 1. Create and save the following three tools: Flat end mill named Rougher with a diameter of 0.5 inches Flat end mill named Finisher with a diameter of 0.25 inches Ball end mill named Ball Rougher with a diameter of 0.5 inches 2. Open the Tools tab of the browser to see the tools listed. 70

72 Version Right-click on the Tools header and select Information. This displays a table listing the properties of all the tools you ve defined. To create the stock: 1. Select Stock / Box Stock. The dimensions of the bounding box are automatically calculated. Change the height to 1.25 from 1.0, so that there will be 0.25 inches of stock material above the part. Do not click OK yet. 2. The stock box is automatically located at the corner of the bounding box, as you can see from the calculated (Xc, Yc, Zc) coordinates. This is the correct location, but for the sake of the tutorial, change the coordinates to (0,0,0). 71

73 Getting Started with VisualMill 3. Click OK. This creates a box that is the right size, but located in the wrong place. 4. To locate the stock correctly, click Locate Part Within Stock on the Machining toolbar. 5. Check Move Stock (so that the stock will move to meet the part) and Bottom so that the bottom face of the stock will align with the bottom face of the part. Check Center to center the stock about the part. 72

74 Version Click Apply to locate the stock correctly. Creating Regions Regions are curves that already exist in your model, or curves you create within VisualMill, using the Curve tools. Regions serve different purposes in 2½ and 3 axis milling. In 3 axis milling, regions are used, when necessary, to define the machining boundary. The center of the tool remains inside the region while following the contours of the part. For example, if you define a region surrounding one surface, only that surface will be milled. In 2½ axis milling, however, regions determine the entire area to be milled. Part and stock geometry are not considered, and the tool always moves at a fixed Z level. Therefore, regions act as the drive curves, and their geometry is projected onto the stock. Regions must be selected (activated) in order to be used in an operation. Creating a region does not make it active; you must use one of the Select Regions tools before creating the toolpath. Note: If a region is not defined for finishing operations, the part silhouette is automatically identified and used as a containment region for the tool. For roughing operations, the stock geometry determines the constraints on the tool location. The Create Regions toolbar contains several tools for creating regions: Each tool is described below: Point: Creates a point by selecting it on screen or entering its coordinates. Points are used as references for other region tools. Mid Point: To create a point at the midpoint of a line, click this icon and select the endpoints of the line. 73

75 Getting Started with VisualMill Center Point: To create a point at the center of a circle, click this icon and then select three points of the circle. Line: Creates a line by selecting two points. Polygon/Polyline: Select the vertices of the polygon. If you want to close the region, move the cursor close to the start point of the region and select it. Right-click to finish. Rectangle: Creates a rectangle by selecting its opposite corners. Circle: Creates a circle by selecting its center and a point on the circumference. Circle by Start Point and Diameter: Creates a circle by selecting two opposite points (diameter endpoints). 3 Point Circle: Creates a circle by selecting three points on its circumference. Arc by Center, Start and Angle: Creates an arc by selecting the arc center, start point, and end point. Arc by 3 Points: Creates an arc by selecting the start point, a point on its circumference, and the endpoint. Auto Chain Edges: Creates a region along a chain of edges. This is useful for creating a region along the outer boundaries of a surface. Select one edge, and all edges in the chain are automatically selected. Manually Chain Edges: Creates a region along a chain you define manually. Select an edge, and a vector will be displayed at the end of the edge. Then select the edge closest to the start of this vector. Continue until either the region is closed, or right-click to finish. Part Bounding Box Region: Creates a rectangular region along the XY plane of the part s bounding box. Stock Bounding Box Region: Creates a rectangular region along the XY plane of the stock box. Undo: Deletes the last point selected to create the region. This is useful when using the Polygon/polyline tool. 74

76 Version 4.0 To create the regions: Because 2½ axis milling does not relate to part or stock geometry, milling regions must be created to define the machining boundaries. 1. Hide the stock, and make sure Hide Regions is not pressed. There are four regions already defined for the part. You can also see the regions in the Geom tab of the browser (not available in VisualMill Basic). These regions are provided so that you can see the regions that need to be defined for the part. We will recreate them manually. 2. Select the Region header in the browser, right-click, and select Delete All Regions. (You could also delete each region individually by right-clicking and selecting Delete, or by dragging a region outside the browser area.) VisualMill Basic users select Edit / Select / Single, press Ctrl, and use the cursor to manually select all four regions. They turn black when selected. Then select Edit / Delete. Note: If you need to redraw the display, select View / Repaint. 75

77 Getting Started with VisualMill 3. If the Create Regions toolbar is not displayed, select View / Toolbars / Curves/Region Bar. This toolbar appears vertically to the right of the screen. 4. Make sure the Osnap indicator is on in the Status Bar. This enables you to snap to points on the part. 5. Select Curve / Chain Edges / Auto Chain Edges, or click the icon on the Create Regions toolbar. 6. With this option, you can select one edge and the entire chain of edges is selected. Use this to create regions around the two chains of edges shown below. Tip: If you obtain the wrong chain (you might select a vertical surface boundary rather than the desired chain), click again in a different place to create the correct region. Then you can simply delete the unwanted region, or leave it if you prefer. 7. The next region is along the circular hole. Select Curve / Circle / 3 Point Circle or select the icon on the Create Regions toolbar. 76

78 Version Select any three points along the top circle to create this region. 9. The final region is a rectangle surrounding the part. Select Curve / Bounding Region / Part Bounding Region or click the icon on the Create Regions toolbar. 10. Because the region should extend slightly past the part extents, enter X and Y offsets of 0.25 inches. 77

79 Getting Started with VisualMill 11. Click OK to create the rectangular region. Selecting Regions Once regions are created in the model, you must select (activate) the regions you want to use in the subsequent toolpath. Region selection tools can be accessed from the Edit / Select menu, or by clicking Select Regions on the Machining toolbar. When selected, a region turns black. Note that any selected regions remain active until deselected, so when you want to activate different regions be sure to deselect any you do not want. The following region tools are available: Single: You can select existing regions by picking them manually. Multiple regions can be selected by pressing Ctrl. Rectangle: Selects all regions within a defined rectangle. Polygon: Selects all regions within a defined polygon. All: Selects all regions defined in the model. None: Deselects any selected regions. 78

80 Version 4.0 Multiple Regions Multiple and nested regions can be selected, but not regions that intersect. When selecting more than one region, keep the Ctrl key pressed. Nested regions are handled according to the following rule: The tool will remain inside an outer region and outside an inner region. A region within an inner region is considered to be an outer region. In the following picture, the shaded areas are where the tool motions occur: Creating Toolpaths Four toolpaths will be created Facing to remove the top layer of stock, Pocketing for the outer and inner areas, and Profiling to finish the holes. To create the facing toolpath: 1. The first step is to activate the region you want to mill. Select Edit / Select / Single, or on the Machining toolbar, click Select Regions, and select Single. This option enables you to manually select one or more regions. 79

81 Getting Started with VisualMill 2. Pick the outermost rectangular region. It turns from blue (the default Wire color, which can be changed in the Color Preferences) to black. Note: In the Regions section of the Geom browser tab, you can see what regions are selected. You can also use the browser to select and deselect regions. 3. Activate the Rougher tool. 4. Select 2½ Axis Milling / Pocketing, or click the 2½ Axis Machining icon on the Machining toolbar and pick the Pocketing option. Note: Because this is supposed to be a facing toolpath, you may be wondering why Facing wasn t selected. We will demonstrate how to make changes later in the exercise. 80

82 Version In the Cut Parameters tab, check the Stock Offset cut pattern, and select the Mixed cut direction. 6. Accept the other default parameters and click Generate. The pocketing toolpath is generated within the defined region. 7. Display the stock, hide the toolpath, and simulate the facing toolpath. This mills to the level of the region, removing the 0.25 inches above the part that was added to the stock box. 81

83 Getting Started with VisualMill The part and regions are displayed in this picture, but you can hide them as well. To create the outside pocketing toolpath: This Pocketing toolpath is similar to the one you just created, and uses the same tool. 1. Hide the stock and make sure the regions are displayed. 2. On the Machining toolbar, click Select Regions, and select Single (as before). 82

84 Version Select the two outermost regions. To select multiple regions, keep the Ctrl key pressed. The tool will move in the area between these two regions. 4. The Rougher tool should still be active. Select 2½ Axis Milling / Pocketing. The Cut Parameters tab should have the same parameters as before (Stock Offset and Mixed). 5. The previous toolpath used the default cut levels, machining to the level of the region, but in this toolpath the cut levels must be specified. Click the Cut Levels tab, check Top and Bottom, and make sure Top is 0.0 and Bottom is 1. 83

85 Getting Started with VisualMill 6. Click Generate. The outer volume surrounding the part is removed. 7. Simulate the toolpath. Clearance Plane The clearance plane is a horizontal plane (set Z level) from which the engage (approach) motions start and retract motions end. After retracting, the tool moves rapidly along this plane to the position of the next engage. This plane is typically a certain safe distance above the part geometry. Clearance levels are set by clicking the Clearance Control button on the Machining toolbar. 84

86 Version 4.0 By default (Automatic option), the clearance level is calculated by adding a safety distance to the highest point found on both part and stock geometry. This safety distance is set to be the current tool radius. You can set the clearance level to be a set distance from either the part or stock, or enter the absolute Z level. To create the inside pocketing toolpath: This pocketing toolpath is almost identical to the outside pocketing, but uses a different tool and different regions. 1. Display the regions and hide the stock. 2. Activate the Ball Rougher tool. 3. For the regions, we want to select the two inner (hole) regions. You can use the same Single method to select the inner regions (pressing Ctrl to select multiple regions), but let s use a different method. Use Select Regions / Rectangle. 85

87 Getting Started with VisualMill 4. Select two points so that the rectangle completely encloses the desired regions. Objects only partially enclosed in the rectangle are not selected. The two inner regions should appear in black. (If the outer regions also appear in black, deselect them with the Single option.) 5. Create a Pocketing toolpath, and leave the parameters as before (Cut Parameters and Cut Levels). Click Generate. The inner pockets are milled. 86

88 Version Turn off the display of the part, so that only the toolpath is visible. You can see the four different types of motions Rapid, Cut, Engage (approach), and Retract. These are color-coded according to the table in Preferences / Color Preferences check these colors if there are motions you cannot see. Engage motions extend vertically from the clearance plane down into the material. Cut motions represent actual cutting of material. Retract motions extend vertically from the material up to the clearance plane. Rapid motions are along the clearance plane. They are fast because there is no danger of collision with material; the clearance plane is set a safe distance above the stock. 7. To change the clearance plane, double-click the Clearance Plane item in the browser for this toolpath. 87

89 Getting Started with VisualMill 8. Switch from the default Automatic to Part Max Z + Dist, and add 1.0 inch. 9. Click OK. In the browser, note that the folder icon for this toolpath is red instead of yellow. This indicates that a parameter has changed, and the toolpath needs to be regenerated. 10. Right-click on the toolpath name and select Generate. 88

90 Version Display the part again. You can see the modified toolpath now uses a higher clearance plane. 12. Simulate this procedure to view the remaining stock. To create the inside profiling toolpath: The final toolpath will profile the inner regions, to bring the stock closer to the desired part. These regions should still be selected from their use in the previous toolpath. 1. Activate the Finisher tool. 2. Select 2½ Axis Milling / Profiling. 89

91 Getting Started with VisualMill 3. In the Cut Levels tab, set Bottom to 1 and change the %Tool Diameter to 10%. This creates a finer toolpath. 4. Click Generate. The profiling toolpath mills around the inner holes. Note: If the toolpath appears on the wrong side of one of the regions, you need to reverse the region direction. Make sure the region in question (and only that region) is selected (black), and select Curve / Reverse. Then regenerate the Profiling toolpath. 90

92 Version Simulate the toolpath. You can compare simulation results by clicking on any operation in the Mops tab of the browser. (It may help to zoom in as well.) If the stock is displayed, clicking a toolpath or any of its components (Stock, Regions, Toolpath, etc.) will show the stock that remains after the toolpath. 91

93 Getting Started with VisualMill Adjusting the Regions You probably have noticed that the second Pocketing toolpath left an undesired piece of stock remaining at the end of the part. This is because the outer region is too close to the part. It was created with a 0.25 offset from the part, but that does not leave enough space for the tool to mill sufficiently around this curve. To increase the region: 1. Select the outer region, making sure all the other regions are not selected. 2. Select Edit / Scale. This will scale all objects currently selected. 92

94 Version Check Uniform Scaling. To increase the size by 5%, change any of the Scale Factor values to The other values update to this value as well. 4. Click Apply to increase the size of the region. 5. Right-click on the second Pocketing toolpath and select Generate. 93

95 Getting Started with VisualMill 6. There is now more room for the tool to move. Simulate to see that the piece of stock is now removed. Replacing the First Toolpath VisualMill Basic users proceed to Modifying Toolpath Parameters. As mentioned above, the first toolpath was created as Pocketing, although it was supposed to be Facing. (The results are the same, but this step illustrates how to delete and replace toolpaths.) To replace the toolpath: 1. In the Mops tab of the browser, right-click on the first toolpath and select Cut. 2. Activate the Rougher tool. 94

96 Version Return to the Mops tab, and make sure the root item is selected, because new toolpaths are inserted below the selected item. 4. Select only the outer region, and make sure no other regions are selected. 5. Select 2½ Axis Milling / Facing and accept all default parameters. Because Cut Levels are not specified, the machining will proceed until the level of the region. 95

97 Getting Started with VisualMill 6. Generate the toolpath. It is placed first on the list. Modifying Toolpath Parameters Once a toolpath is created, you can go back and change any of its parameters. This example will include two simple changes to the inner pocketing toolpath. To modify the toolpath parameters: 1. In the second-to-last toolpath, double-click Regions and select Single. 96

98 Version Deselect the circular region. Now only one region (the long one) should be selected (shown in black). Note that the folder icon for this toolpath is red indicating that something has changed and the toolpath must be regenerated. 3. Now double-click Cut Parameters for this toolpath. 97

99 Getting Started with VisualMill 4. Change the Cut Pattern to Linear. This changes the pattern from a spiral pattern to a series of parallel cuts. 5. Click Generate. The modified toolpath is now only in one region, and has a linear pattern. 98

100 Version 4.0 Toolpath Editing Not available in VisualMill Basic. Basic users proceed to Tutorial 3. Once a machining operation is created, the toolpath can be graphically edited and post-processor commands can be added. The Toolpath Editor provides many useful tools, a few of which will be demonstrated here. The editing will be done on the same toolpath you just modified the pocketing on the inner region. To edit the toolpath: 1. First, hide everything but the toolpath. 2. Double-click on the Toolpath icon in the browser for this toolpath. 99

101 Getting Started with VisualMill (Another way to open the Toolpath Editor is to click Toolpath Editor on the Machining toolbar.) The Toolpath Editor opens to the right of the screen. You can move it by dragging one of its corners. Each line is a line of the G-code that will be sent to the machine. At the bottom is the operation name, number of GOTO s (tool motions), and estimated machining time. 3. Place the cursor in one of the numbered lines, and use the arrows to move up or down. For the lines that represent tool motion, the tool will appear to indicate how it moves on that particular line. 100

102 Version We will now change some of the movements. Click Select motions inside rectangle. 5. Click two points to define a rectangle that encloses some of the tool motions. 6. All of the motions, and portions of motions, within the rectangle are selected. Click Cut Selection. 101

103 Getting Started with VisualMill The motions inside the rectangle are deleted, and engage / retract motions are added to accommodate the new toolpath. 7. To restore the toolpath, click Reset Toolpath. (You can also regenerate the toolpath using the browser.) 8. Draw another rectangle to select tool motions in the center of the toolpath. 102

104 Version Click Isolate Selection All motions other than those selected are deleted. 10. Restore the toolpath, and use another rectangle to select motions near the top. 103

105 Getting Started with VisualMill 11. Click Move Up/Down Selection. 12. Move all selected motions by a DeltaZ of 1.0. The selected motions move up by 1 inch. 104

106 Version Restore again, and click Transform Toolpath. This tool enables you to move, rotate, or scale the toolpath, and optionally make copies of it. 14. Click the Rotate tab, and rotate the toolpath 90 degrees about the Z axis. Click Apply. 105

107 Getting Started with VisualMill The toolpath rotates 90 degrees. The final editing we will demonstrate is instancing. This means creating multiple copies of a toolpath, either in an XY array or in Z levels. 15. Restore the toolpath and click Instance Toolpath. 106

108 Version For the array, specify an X and Y spacing and numbers in X and Y as shown below. (This uses the Spaced method; in the Fitted method you fit a number of copies evenly in a specified total distance.) 107

109 Getting Started with VisualMill 17. Click OK, and there are now six toolpaths. You will probably have to zoom out to see them all, or use Fit View. End of Tutorial 2! (Obviously you wouldn t leave your toolpaths in this condition, but we ll assume it s OK for the purposes of the tutorial.) 108

110 Version 4.0 Tutorial 3: Drilling Operations This exercise will help you understand and use the drilling module in VisualMill. The following types of drilling operations are available: Drill: Standard, Deep, Break chip, Counter Sink Tap (Not available in VisualMill Basic): Clockwise, Counter Clockwise Bore (Not available in VisualMill Basic): Drag, No Drag, Manual Reverse Bore (Not available in VisualMill Basic) To set up the file: 1. Load the part file, RouterBitHolder.vmp. 2. Create a Part Box stock with zero offsets. 109

111 Getting Started with VisualMill To drill the larger holes: 1. Click the Tools tab in the browser. There are several tools that have already been created in this file. The first two have already been used in toolpaths. 2. Double-click on DrillTool1 to open the window in which it was created. This is one way to verify and edit a tool s parameters. 3. Double-click on the tool name to activate it. 4. The next step is to select the regions to be drilled. Make sure the regions and part are displayed. 110

112 Version All of the large holes are to be selected first. Open the Geom tab of the browser and expand the Regions. VisualMill Basic users - switch to top view and use Select Regions / Rectangle as you did in the previous exercise. Select two points to define a rectangle enclosing all the regions around the large holes. Then proceed to Step On the Machining toolbar, select Regions / Single. 7. On the Geom tab, use Shift to select the first 24 regions (the 24 larger holes). These holes are indicated in black. 111

113 Getting Started with VisualMill 8. Select Drilling / Drilling, or click Drilling on the Machining toolbar and select Drilling. 9. The Drilling window appears, in which you can set Cut and Engage / Retract parameters. This window can be used to perform Standard, Deep, Break Chip or Counter Sink drilling. For now, leave the parameters at their default values. 112

114 Version Click Generate. Note: Depending on the part color and colors of tool motions, some of the motions may be hard to see. You can change these colors by selecting Preferences / Color Preferences. To drill the smaller holes: 1. Activate the smaller tool - DrillTool2. This tool has a diameter of 0.25 inches. 2. Select Regions / None to deselect the larger regions. Then use the method you used before to select the 18 small regions. 3. Generate another Drilling toolpath on these holes. 113

115 Getting Started with VisualMill 4. Display the stock, hide the part and toolpaths, and simulate the toolpaths. You can proceed to use the same part to generate Tap, Bore and Reverse Bore toolpaths. 114

116 Version 4.0 Not available in VisualMill Basic Creating Fourth Axis Toolpaths Tutorial 4: 4 th Axis Machining Operations This exercise uses fourth axis machining operations to machine a two-sided part. Fourth axis machining is considerably more complex than 2½ and 3 axis machining, and requires thorough understanding of the machining process. You should be very familiar with aspects of 3 axis milling before working this exercise. Load the part file Flashlight.vmp. Cutting Strategy This part cannot be completely machined using only one set of 3 axis operations. We will divide the part geometry into two sections, by creating a parting plane through the middle of the part. Then we will cut the top half first, flip the part over and cut the bottom half. We first need to determine how the part will be held in the machine. In this exercise we will hold the part so that the axis of the part geometry is aligned with the X axis of the machine coordinate system. 115

117 Getting Started with VisualMill We next need to determine which areas of the part will not be machined. Some areas of the part must remain un-machined to prevent the part from falling out of the stock material. In addition, if there is not sufficient material joining the part to the raw stock material, the part may move during machining. In this exercise we will initially keep the ends of the part in the stock geometry. These ends will have to be cut away afterward to obtain the final finished model. Measurement Toolbar One of the steps in the next part of this tutorial is to measure the part. Measuring tools can be found on the Measure menu and on the Measurement toolbar (View / Toolbars / Measurement). When a measurement is calculated, it is displayed in the bar at the top of the screen. Vertex Coordinates: Displays XYZ coordinates of a selected point. Measure Distance: Measures the distance between two points. The point coordinates and the distance between them will be displayed. Measure 3 Vertex Radius: Measures the radius of an arc spanning 3 points. The point coordinates and their arc radius will be displayed, and the arc will appear temporarily. 116

118 Version 4.0 Part Bounding Box: Calculates the dimensions of the bounding box around the part. Part Center: Calculates the coordinates of the center of the part. Setting the Machine Zero For parts be machined using the rotary axis, it is recommended that the machine zero be located on the axis of rotation of the part geometry. To set the machine zero: 1. Display the coordinate axes and the grid, so that you have a clear picture of the part s orientation and location. You can see that the part is not centered in the Z direction. 2. Display the Measurement toolbar and click Part Center. Or select Measure / Part Center Coordinates. 117

119 Getting Started with VisualMill This verifies that the part is centered along X and Y, but not along Z. 3. Click Set Machine Zero on the Machining toolbar. 4. Select Set to Part Box, Mid Z, and Center. This places the machine zero at the center of the part. Click Apply. 118

120 Version Measure the part center coordinates again. Now the part is centered in all three directions. Setting the Rotation Axis VisualMill assumes that the part is located on a rotating table, and that the table can rotate about either the X (A) axis or the Y (B) axis. You need to specify the rotation axis and the rotation center point. It is recommended to align the machine s rotation axis with the natural rotation axis of the part. To set the rotation axis and center: 1. Select 4 th Axis / Set Table Rotation Params, or click Table Rotation Params on the Machining toolbar. 119

121 Getting Started with VisualMill 2. Select the A Axis, and specify (0,0,0) for the rotation center. The axes are at the center of the part, but the grid is no longer centered. This is because the grid is currently a set Z elevation relative to the origin, as you will see in the next step. Because we will need to use the grid to create the parting surface, the grid needs to be moved to the part center. Creating the Parting Plane We will first use 3 axis operations to rough this part, in which the tool can only move in the Z direction. For parts like this, objects should be divided into top and bottom sections. Then the top half can be milled, followed by the bottom half. A parting plane will be used to separate the part into two machinable sections. 120

122 Version 4.0 To create the parting plane: 1. We need to adjust the grid, but first we need to measure the part to determine the grid spacing. Select Measure / Part Bounding Box. The flashlight is long. 2. Select Preferences / Grid Preferences. On the opening tab, enter the spacings as shown below. The Grid Spacing value (0.3125) is a divisible factor of the part length, ensuring that there will be grid lines flush with the ends of the part. 121

123 Getting Started with VisualMill 3. Click the Set Grid Elevation tab. The Elevation is set to 0.75, which explains why the grid is located below the origin. 4. Click the Set Grid Center tab, and change the grid origin to (0,0,0). Note: You also could have done this in the Set Grid Elevation tab, by clicking Part and Center. 122

124 Version 4.0 The grid is now centered along the part. 5. Create a Part Box Stock with zero offsets. 6. Make sure the Snap indicator is on in the Status Bar, so that you can snap to grid points. 123

125 Getting Started with VisualMill 7. Select Curve / Line / Rectangle to create a rectangular region. Select two corner points so that the rectangle surrounds the part and is flush with the ends. This region represents the parting plane. Tool motions cannot extend past the region, and because the region is flush with the ends, the ends of the part will not fall out of the stock. 8. Select this region to activate it. It is easier to see if you hide the grid. 124

126 Version 4.0 Creating 3 Axis Roughing Toolpaths The toolpaths can now be created. The strategy is to first rough the top half of the part, then rotate the table180 degrees to expose the bottom half. The bottom half will be roughed, and then finish operations will be performed. To create the roughing toolpath for the top half: 1. Create and save a ball end mill with a 0.25 inch diameter. This tool will be used for all toolpaths. (There is already a ball end mill in the file; you can edit this tool to have the correct diameter.) 2. Reset the Clearance Plane to Automatic. 3. Select 3-Axis Milling / Horizontal Roughing. In the Cut Parameters tab, select Stock Offset so that the motions will be contained inside the region. Select Mixed to minimize retract motions. 125

127 Getting Started with VisualMill 4. For Cut Levels, set Bottom to zero so that the machining stops at the parting surface. 5. Click Generate to rough the top part. 126

128 Version Simulate the machining so far. Now the part needs to be flipped, to expose the bottom half. This will be done by rotating the table 180 degrees. In VisualMill, this is done as a machining operation. To rotate the table: 1. Select 4 th Axis / Rotate Table, or use the 4 th Axis icon on the Machining toolbar. 127

129 Getting Started with VisualMill 2. Enter a rotation angle of 180 degrees. 3. Click Generate. A Rotate Table machining operation appears in the Mops tab of the browser. Note: The display of the part does not change as a result of the table rotation. In reality, however, the machine would have turned the table. 128

130 Version 4.0 To create the roughing toolpath for the bottom half: Because the roughing for the bottom half will have the same parameters as the roughing for the top half, we can copy and paste the toolpath. 1. Right-click on the first toolpath (Horizontal Roughing) and select Copy. Or select the toolpath and press Ctrl+C. 2. The second roughing operation needs to go after the Rotate Table operation, so right-click on that toolpath and select Paste. Or use Ctrl+V. 129

131 Getting Started with VisualMill 3. The toolpath is copied, but its icon is red, indicating it needs to be generated. Right-click on it and select Generate. The toolpath is displayed on the bottom of the part. Since VisualMill does not actually alter the part geometry in the display after the Rotate Table operation, this is how you know the correct side is being machined. 130

132 Version Simulate the toolpaths so far. If you are still running the 3 axis simulation model, you will receive a message that rotated toolpaths cannot be handled. Click Yes to switch to the 4 axis simulation model, and you will have to simulate all toolpaths from the beginning. Note: As described earlier, the standard VisualMill product has two material removal simulation modes (or models). The 3 axis model can only be used for 2½ and 3 axis toolpaths. The main advantage of this model is very rapid processing times. The 4 axis model is necessary for simulating all 4 th axis toolpaths. This model is more comprehensive and results in better display quality, at the expense of speed. You can set the simulation model by selecting Preferences / Machining Preferences. Creating 4 th Axis Indexed Mode Finishing Operations Once the rough machining is performed, you have the option of finishing the part in either indexed (locked table) or continuous (tool motions normal to table rotation) 4 th axis mode. For roughing, the recommended method is always indexed mode. When the table is in a locked position, as it is during indexed mode machining, it is at a much more rigid state. This allows for heftier cuts and therefore higher rates of material removal. Indexed mode finishing can be used if all features of the part can be accessed completely during this type of machining. If any features are completely or partially inaccessible to the tool during indexed mode machining, the machining will be incomplete and you should use continuous machining. We will examine both methods, starting with indexed mode. Remember that the rotation table is already at an indexed position of 180 degrees. So we will first finish the bottom half, and then the top half. Finish machining can be performed by Parallel Finishing machining. 131

133 Getting Started with VisualMill To create the finish toolpaths for both halves: 1. Deselect all regions. The Parallel Finishing method will automatically detect parting planes, as well as the extents of part geometry. 2. Select 3 Axis Machining / Parallel Finishing. The parameters are already set to finish tolerances. Set Stock thickness to 0, and specify Stepover = 10% of the tool diameter. 132

134 Version Click Generate. The toolpath is created on the bottom half, which can be better seen if you rotate the part slightly. 4. To flip the table back, create another Rotate Table operation, using a rotation angle of 0 degrees. 5. Make a copy of the Parallel Finish operation after the Rotate Table operation, and Generate it. This time the top half is machined. 6. Simulate these finish toolpaths. 133

135 Getting Started with VisualMill Note the ridge of unremoved material at the parting plane. This is present because a ball end mill tool was used. To remove this ridge, the tool has to go below the parting plane by the length of the tool radius. You could also avoid this problem by using a flat end mill, but this might not be appropriate for finishing. You could also use more than two table rotations, or use continuous mode finishing to remove the ridge. As mentioned before, indexed mode finishing can be used effectively only if all features can be accessed completely, which is not exactly the case in this example. 134

136 Version 4.0 Creating 4 th Axis Continuous Mode Finishing Operation In continuous machining, tool motions are always normal to the axis of table rotation; the table rotates constantly rather than flipped once or twice. This type of machining is especially suitable for machining jewelry such as rings and bracelets. Roughing operations should still use indexed mode. To create the continuous finishing operation: 1. The previous three finishing operations should be deleted. You can right-click on each one and select Cut, or use Shift or Ctrl to select all three, right-click and select Delete All. 2. Select the last Horizontal Roughing operation, so that the new finish toolpath will be created after it. 135

137 Getting Started with VisualMill 3. Select 4 th Axis / 4 th Axis Parallel Finishing. In the Cut Parameters tab, make sure the remaining Stock thickness = In the Step Control tab, enter 10% of the tool diameter. 5. Click Generate. Because this is such a fine toolpath, it may take a few minutes to complete. 136